The Designer's Guide Community Forum

The Designer's Guide Community Forum
https://designers-guide.org/forum/YaBB.pl
Design >> Analog Design >> Help with spectreRS for SC-CMFB
https://designers-guide.org/forum/YaBB.pl?num=1071672270

Message started by Count on Dec 17^th, 2003, 6:44am

Title: Help with spectreRS for SC-CMFB
Post by Count on Dec 17^th, 2003, 6:44am

I have a differential opamp using SC-CMFB ckt and I would like to see the DCOP and the AC analysis. I found out that to do so I would need to use the PSS, PAC and PXF analysis priovided by spectreRF. However, I really do not know how to perform the test. Please help. THanks

Title: Re: Help with spectreRS for SC-CMFB
Post by Ken Kundert on Dec 17^th, 2003, 8:12am

Apply the clock only and run a PSS analysis. The PSS analysis will play the role of a DC analysis for a traditional amplifier. It computes the operating point, but rather than computing a simple DC operating point, it computes a "periodic operating point", with the period being that of the clock.

Then perform a PAC analysis to compute the transfer functions. The PAC analysis plays the role of an AC analysis for a traditional amplifier. To do so, start by setting pacmag=1 on some source. The start and stop frequency you specify on the PAC analysis define the frequency sweep range for this source. The PAC analysis computes the transfer function from that source to every node in the circuit. Because the clock is present, there will also be frequency conversion effects present. PAC can also compute the transfer functions from the source frequency to any sideband frequency f = k*f_o, where f_o is the clock frequency and k is an integer. You probably are interested in output signals that are at the same frequency as the input frequency, so you would observe sideband k=0.

I recommend reading the paper "Simulating switched-capacitor filters with SpectreRF" at www.designers-guide.com/Analysis/.

-Ken

Title: Re: Help with spectreRS for SC-CMFB
Post by Count on Dec 17^th, 2003, 9:25pm

I tried to do a PSS analysis and there are some of the questions I want to ask. Is it possible to see all the node voltages on the schematic itself rather than plotting out the voltage of each node? Thanks

Title: Re: Help with spectreRS for SC-CMFB
Post by Ken Kundert on Dec 17^th, 2003, 11:01pm

I don't believe so. Artist only back-annotates the DC voltage (as computed by the DC operating point) to the schematic. I believe that you want to see the DC component of the node voltages as computed during the PSS analysis.

-Ken

Title: Re: Help with spectreRS for SC-CMFB
Post by Count on Dec 18^th, 2003, 6:19am

Thanks for your rapid reply.
I hope I don't really bother you too much. One more question i.e. how do I test the configuration in figure 1 of http://www.dessent.net/resume/ee240-dessent.pdf ?

I tried using transient analysis but I guessed this is not the right way. Please enlighten me. Thanks a lot.

Title: Re: Help with spectreRS for SC-CMFB
Post by Ken Kundert on Dec 18^th, 2003, 1:53pm

The difficulty with that circuit is that in order to apply SpectreRF the analysis must occur about a steady-state solution. The circuit you are analyzing has no DC feedback, and so in practice the voltages on the input terminals will drift until they leave the compliance range for the amplifier. In order to analyze the circuit with SpectreRF, you will need to provide some form of feedback for DC signals. The feedback can be in the form of very large resistors, or it can be in the form of switched-capacitor resistors.

Once you modify the circuit so that is has a steady-state response, then you can apply the PSS analysis followed by what ever small-signal analysis you are interested in.

-Ken

Title: Re: Help with spectreRS for SC-CMFB
Post by Ken Kundert on Dec 20^th, 2003, 2:32pm

Here is the basic circuit ...

There is nothing in this circuit that sets the DC differential input level. Only capacitors are connected to the inputs of the opamp, and so DC input level is free to drift. And because the opamp is a high-gain amplifier, and offset on the input will cause the output to drift much faster. The drift on the input is often so small as to be unnoticeable, but the drift on the output can be substantial. Soon the amplifier drifts out of its proper operating region.

Having switched-capacitor common-mode feedback (SC-CMFB) aggravates this situation by injecting charge into the system that can cause the drift. This problem can be made even worse by the simulator itself, because it does not completely conserve charge (there is a section in my book about this). HSpice is notoriously bad at this. With Spectre you can dramatically reduce the charge error without slowing down the simulations much be tightening reltol by a factor of 10-100 while simultaneously loosening lteratio by the same factor. (reltol is a global simulator options, lteratio is an option of the transient and PSS analyses).

Tightening the tolerance acts to reduce the problem, but it does not eliminate it. The basic issue is that this circuit is not viable. If it were placed on chip as is, it would not take very long before charge would build up on the inputs and the amplifier would stop working. To eliminate the problem completely means that some way must be provided to properly fix the DC operating conditions at the input of the amplifier. Clearly this amplifier is sitting in a test bench consisting of capacitors and voltage sources that is meant to "represent" the rest of the circuit. Well, an important piece was left out, the DC biasing. Somehow that aspect of the circuit must be included in the test bench.

There are a two basic ways of performing these simulations. The first is to simply force the circuit to the right operating point using switches, initial conditions, etc. and then hope it stays there long enough for you to make your measurements. For example, you can use the "switch" component in Spectre and configure it so that it forces the DC operating point in the DC analysis but opens up in AC or transient. Or you can set the operating point using initial conditions, perform a brief transient analysis, and then follow it up with an AC analysis with "prevoppoint=yes" set so that it performs the analysis using the last transient point as the operating point.

The other way is to include the DC biasing aspect of the larger circuit into the test bench. Presumably this involves more switches and clocks. Then you can use SpectreRF to perform the small-signal analyses and transient to predict slew rate and settling time.

-Ken

Title: Re: Help with spectreRS for SC-CMFB
Post by Count on Dec 23^rd, 2003, 6:21am

Hi Ken, I still do not quite get it. Within the opamp itself, there's a dyanmic CMFB that forces the output DC to be the value I wanted. I have tried PSS and found out that the DCOP is indeed as expected. I use PAC to find out the open loop frequency response and it was as expected too. However, when I tried to perform the transient response, it just won't work.

I have tried the second method you mentioned but the transient analysis still failed. Correct me if I am mistaken, I could just do a transient analysis directly to find the settling time, right? Thanks

Title: Re: Help with spectreRS for SC-CMFB
Post by Ken Kundert on Dec 23^rd, 2003, 9:16am

When you say that transient analysis failed, do you really mean that it failed? Or do you mean that you did not get the result you expected? I expect it is the latter, which implies that transient analysis is telling you something about your circuit that you did not know.

The low frequency feedback in your circuit only applies to the common-mode signal. And as you point out, the common mode signal is not drifting off. It is the differential mode signal that it drifting. It is differential feedback you need to apply at DC.

-Ken

Title: Re: Help with spectreRS for SC-CMFB
Post by The_One on Dec 25^th, 2003, 6:38pm

Ken Kundert wrote on Dec 20^th, 2003, 2:32pm:

Here is the basic circuit ...

The other way is to include the DC biasing aspect of the larger circuit into the test bench. Presumably this involves more switches and clocks. Then you can use SpectreRF to perform the small-signal analyses and transient to predict slew rate and settling time.

-Ken

Hi Ken,

I am interested in your statement above. Would you mind to tell me what kind of larger circuit I need to use?

Thanks a lot.

Title: Re: Help with spectreRS for SC-CMFB
Post by Ken Kundert on Dec 26^th, 2003, 7:47am

There must be something in the larger circuit that provides differential DC feedback to the circuit. It could be large value resistors in parallel with the feedback capacitors, but more likely it is some switching network, such as auto-zero switches across the feedback capacitors or a switched-capacitor resistor that provides the feedback.

-Ken

Title: Re: Help with spectreRS for SC-CMFB
Post by The_One on Dec 26^th, 2003, 9:41am

Thx Ken.
I will try it out.

Title: Re: Help with spectreRS for SC-CMFB
Post by Rave on Sep 25^th, 2004, 2:45pm

Hi ken

I m using cadence icfb tool for running simulations with the NCSU kit, as u said above in order to run pac simulation we need to set pacmag=1 on one of the source. How do I do that, i tried setting AC magnitude on a simple DC voltage source as 1 but seems like that is not helping with the pac magnitude.

thanks

Title: Re: Help with spectreRS for SC-CMFB
Post by Andrew Beckett on Sep 26^th, 2004, 2:49am

There is a separate parameter on the sources called
"PAC magnitude". You're better off using the vsource component in analogLib which can be configured to be any kind of source (including dc), and has a toggle "display small signal parameter" (or something like that) which will then show up PAC Magnitude (either in volts or dBm)

Andrew.

Title: Re: Help with spectreRS for SC-CMFB
Post by Rave on Sep 26^th, 2004, 11:50am

Thanks Andrew

But I dont see any such component in my library, the analog library has a library voltage_sources which has the sources as ccvs, vcvs, vdc, vexp,vpulse,vpwl,vsin.

If i choose vdc, then the parameters are 'AC magnitude' 'AC phase' 'Noise' 'Temperature Coeff 1' 'Temperature Coeff 2'.

I dont think this 'AC magnitude' is 'pac magnitude'.

Is there any other way to get around this problem??

Thanks

Title: Re: Help with spectreRS for SC-CMFB
Post by Frank Wiedmann on Sep 27^th, 2004, 4:43am

There should be a library named analogLib where you will find the vsource component that Andrew mentioned. If you do not have access to this library, you should ask the people responsible for your Cadence installation to make it available.

Title: Re: Help with spectreRS for SC-CMFB
Post by Andrew Beckett on Sep 29^th, 2004, 7:57am

Or you may be using a version prior to IC445 which is when vsource
was introduced in analogLib. You could use psin, but that has a port impedance.

There may be other sources that have pac magnitude prior to IC445, but I can't check quickly at the moment.

You may just be pointing at an old copy of analogLib, as Frank mentioned?

Andrew.

Title: Re: Help with spectreRS for SC-CMFB
Post by Rav on Sep 29^th, 2004, 4:38pm

@ Frank
In my previous post thats what I specified that there exists an analog lib and i specified the components too, but the problem is there doesnt exist any component like vsource. As far as I know we are using NCSU CDK 1.3 kit.

Very likely I am using the old library, but its not easy for me to get it changed, is there any way to get around this problem, i mean can i create a netlist without vsource and then add a vsource in the netlist manually and simulate netlist????

Also i checked that their does exist psin but it does not have pac too, it has : resistance, port number, DC voltage, sine DC level, amplitude, phase, frequency, FM index, AM index, AC magnitude and AC phase.

There is similarly a pdc component too, and that has resistance, port number, DC voltage, AC magnitue and AC phase but here i think p refers to port not to periodic.

Thanks

Title: Re: Help with spectreRS for SC-CMFB
Post by Frank Wiedmann on Sep 30^th, 2004, 12:17am

In current versions of the library analogLib, you will find the parameters PAC magnitude and PAC phase in all independent sources. If you have absolutely no possibility to get access to this library, you might be able to work around this problem by using include files. However, as I do not know the details of your Cadence installation, you should discuss this issue with your local experts in order to find the best solution.

Title: Re: Help with spectreRS for SC-CMFB
Post by jbdavid on Nov 1^st, 2004, 5:51pm

One of the problems with the NCSU kit is that they used an old version of analogLib from the cadence install, so that they could give instructions on using it with out it changing in the next version of the tools..

What you need to do is look in the cadence documentation for the location of analogLib, and add that to your library instead of the NSCU one.. rename the NSCU one if needed. the NCSU folks probably didn't consider the use of SpectreRF in analog design.

A better tutorial design kit, one that is close in architecture to those provided by real foundries is the cadence generic Process Design Kit (PDK). I believe the website for the university programs that are using this as the core of a tutorial program is http://crete.cadence.com
you should be able to register there, and download that kit once your registration is approved.

Hope this helps,
JBD